BACK COUNTERBORING HELP

[bhayden10]

I have a job that requires a back spotface operation and I have never done this and not sure how to. I plan on using a tool like vermont tool sells that uses an insert so i will have to move off center of the hole, plunge down, move over to center and then cut up to a depth of .032. I would be most appreciative if someone could help me with this.

Thanks in advance!

[Guest]

Brian,

 

If you do a search, I believe it crazymillman or maybe James, I forget, that had a macro and/or a custom drill cycle to do just this.

[Psychomill]

What machine and control are you using? Many machines have canned cycles to do this which you can set up in MC as a custom cycle for back boring. Typically the code is a G87 (Fanuc). Mazaks have G87 as well as a G77.....

 

You might have code set up like this:

 

G87G98X??Y??Z-.5R-.6Q.08F10.

 

Where...

"Z" = the cutting depth relative to the work offset 0

"R" = the clearance plane below the c'bore

"Q" = the shift amount for the tool to clear the thru hole.

 

Also you can add "P" for a dwell and "K" for repeats.

 

Generally, a parameter control the direction of shift for "Q". It can be either in the X +/-, or the Y +/- directions. Some machines can also be set to shift in both X and Y directions...

 

 

[bhayden10]

Morning John! I can always count on you. I actually have done searches already for counterboring and back counterboring but nothing like this came up. Any ideas what else i could search under?

Thanks

[bhayden10]

Psycohomill,

I have a 2005 haas vf6. So this may require some manual programming then huh?

[Psychomill]

No, on a Haas, you have a canned cycle. You should be able to use a G77 like this:

 

G77G98X??Y??Z-.5R-.6Q.08F10.

 

Additionally, the "Q" is an incremental shift amount. I also can't recall the parameter that control the shift direction on a Haas. I would just try out this code on the machine but stay way above the part and watch it go through the motions so you know which direction the cutting edge needs to be facing to clear the thru hole...

 

[htm01]

look up g77 in your haas manual,if you don't have it, i could scan it

[terry5357]

BEEEEE careful that you correctly orient the tool so it clears the side of the hole instead of crashing into the face of the part. I had to use G76 (on a H. mill) for fine boring, I had an operator who didn't pay attention when he was setting up for these parts, and destroyed not one but 2 Iscar micro adjust boring heads.

 

Haas is pretty good about meeting the demands of the machining world, I would put money on it having that canned cycle.

[bhayden10]

Thanks a bunch for the help guys, i'll go check it out now and see if it does.

[desmotom]

We use a tool that when it is turn counter clockwise it unlocks the cutter and it swings out and then retract after cutting ..... can't remember what they're called??

[Guest]

quote:

---

Haas is pretty good about meeting the demands of the machining world, I would put money on it having that canned cycle.

---

Spoken like someone who's never run a "real" machine

 

[crazy^millman]

I did a custome drill cycle to do this, but it is the removeable type becuase we are doing really stupid back counterbore. The last one was a 1" back spot face for a .31 d hole. We reamed it with a .251 reamer and then used a .250 polit. You pick the point with the program. It spits out all of the codes to stop the spindle and everything. When I get home I will see if I can dig it up for you.

[Keith @ Solid Code Solutions]

quote:

---

Spoken like someone who's never run a "real" machine

---

Here Here!

[Fig sign]

You can always easy write it by hand using local call code .

In Okuma it was MCALL .

Exists for fanuc and any other

[nathaninc]

Mr. 5Axis C.G. Can you paste that custom drill cycle for us?

[crazy^millman]

Sorry on vacation will have to wait till I get back.